topic Re: Struggle with annotating angle dimension in drawing. in Inventor Forum

Struggle with annotating angle dimension in drawing

Anonymous — Wed, 28 Dec 2016 14:32:07 GMT

I am struggling with annotating angle dimensions in drawing view using Autodesk Inventor Professional 2017.

The part in my drawing is a circular disk with 16 holes close to the edge, 20 degrees apart. When I am trying to annotate the angle, using dimension,from hole to hole, nothing is happening. I have also tried to create a sketch with the part projected, with lines illustrating the angle without any luck.

The only way I can accomplish angle annotation is to create a non-projected sketch, where I draw the angle lines on free-hand, which is quite bothersome.

There has to be a lack of functionality I am missing here, have anyone experienced the same?

Thanks

Re: Struggle with annotating angle dimension in drawing

TheCADWhisperer — Wed, 28 Dec 2016 14:56:10 GMT

Attach your files here.

I will wager that the solution is easy.

I certainly wouldn't do a "freehand" sketch.

Re: Struggle with annotating angle dimension in drawing

SBix26 — Wed, 28 Dec 2016 15:40:23 GMT

Sounds as if you just need to use the Centerline tool to make a "bolt circle" through those holes. This will provide properly oriented center marks at each hole that you can use for angle dimensioning.

Sam B

Inventor Professional 2017 R3
Vault Basic 2017.0.1
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

Re: Struggle with annotating angle dimension in drawing

Anonymous — Thu, 29 Dec 2016 06:35:55 GMT

Still struggling.

Here's a when I try getting the dimension. It just turns blue and does nothing.

I have attached the files.

Re: Struggle with annotating angle dimension in drawing

Mark.Lancaster — Thu, 29 Dec 2016 13:56:57 GMT

@Anonymous

As @SBix26 pointed out you need to use the center pattern annotation centerline. No need to create a sketch..

However there's something wrong with your drawing view because even when I did the proper annotation it still didn't work. So I recreated your base view in your drawing and its now work.

Also just wondering why your view orientations (related to the view cube) are kind of messed up. Meaning your base view in the drawing is based on a bottom view. In my opinion its not really modeled correctly.

Re: Struggle with annotating angle dimension in drawing

Anonymous — Thu, 29 Dec 2016 14:14:20 GMT

Hi, thanks for your answer.

I have realized that this problem is present in some drawings. Do you have any idea what causes this?

And you have right, when I try to create a new drawing it works perfectly to assign angle dimension.

Is this a bug or is it a setting for avoiding this?

About the "bottom-top" comment, does this matter when the bottom is identical with the top?

Re: Struggle with annotating angle dimension in drawing

Mark.Lancaster — Thu, 29 Dec 2016 14:51:23 GMT

@Anonymous

I guess looking at home position of the view cube, too me Its just an odd orientation. I come from board drafting days and my base or primary view would never be based on a bottom view of a part or assembly. Same with CAD, my primary view would most likely be based on a front view. Anyhow my 2 cents..

Re: Struggle with annotating angle dimension in drawing

blandb — Thu, 29 Dec 2016 16:22:53 GMT

Don't forget you can right click on the view, and select "Automated Centerlines". This works for normal views and will place the circular pattern for you. It also works for side view to place in the center line.

But if you ever change your pattern, your drawing will break. Please see link below:

https://forums.autodesk.com/t5/inventor-ideas/automated-centerlines/idi-p/5247915

It has been accepted, was hoping to see it in an update..maybe next release.

Hope this helps!

Re: Struggle with annotating angle dimension in drawing

Anonymous — Tue, 02 Oct 2018 15:28:21 GMT

I had same problem when dimension angle for ladder with cage. One of my college finally solved this problem by changing " general dimension type" to " projected" instead of " true".

right click mouse and choose " general dimension type".

Re: Struggle with annotating angle dimension in drawing

Anonymous — Tue, 02 Oct 2018 18:48:08 GMT

@Mark.Lancaster wrote:

However there's something wrong with your drawing view because even when I did the proper annotation it still didn't work. So I recreated your base view in your drawing and its now work.

I'm unable to download the part and drawing but I'm just wondering if his view is ever so slightly skewed and thus causing the issue? Just a thought.

But yes, draw the centerlines in as shown and then just dimension centerline to centerline.

Re: Struggle with annotating angle dimension in drawing

SF8906 — Fri, 29 Mar 2019 20:40:15 GMT

Re: Struggle with annotating angle dimension in drawing.

Anonymous — Mon, 18 Nov 2019 10:34:57 GMT

Right click on model ---> General Dimension Type ---> Click on Projected